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Problems with Extruding in FeatureScript

3966_cad3966_cad Member Posts: 10 EDU
var sketch1 = newSketchOnPlane(context, id + "sketch1", {
                "sketchPlane" : plane(vector(0, 0, 0) * inch, vector(0, 0, 1))
        skRectangle(sketch1, "rectangle1", {
                    "firstCorner" : vector(0, 0) * inch,
                    "secondCorner" : vector(1, 2) * inch
        skRectangle(sketch1, "rectangle2", {
                    "firstCorner" : vector(0.1, 0.1) * inch,
                    "secondCorner" : vector(0.9, 1.9) * inch
        debug(context, sketch1);

        var origin is Vector = vector(0, 0, 0) * inch;
        var extrusion1 = qContainsPoint(qSketchRegion(id + "sketch1"), origin);
        opExtrude(context, id + "extrude1", {
                    "entities" : extrusion1,
                    "direction" : evOwnerSketchPlane(context, { "entity" : extrusion1 }).normal,
                    "endBound" : BoundingType.BLIND,
                    "endDepth" : definition.length * inch
        debug(context, id + "extrude1");
I am trying to code in FeatureScript to generate a part for an assembly to save me the hassle of importing the part and so on. However, I am running into an error: 
"Call qContainsPoint(Query (map), boolean) does not match qContainsPoint(..., Vector)"
I am trying all types of things to solve this, but nothing is working. It would be very helpful if someone could tell me what is wrong with my code.


  • ilya_baranilya_baran Onshape Employees, Developers, HDM Posts: 1,125
    I can't reproduce the problem -- when I paste your code (with a length parameter) into a feature studio, I get an extruded frame, as one would expect.  A link to your document would help diagnose what's going on.
    Ilya Baran \ VP, Architecture and FeatureScript \ Onshape Inc
  • 3966_cad3966_cad Member Posts: 10 EDU
    Got it
  • ilya_baranilya_baran Onshape Employees, Developers, HDM Posts: 1,125
    Ok, I'm seeing a different problem than the one you reported:
    qCreatedBy(sketch1, EntityType.FACE)<br>
    should be
    qCreatedBy(id + "sketch1", EntityType.FACE)

    Ilya Baran \ VP, Architecture and FeatureScript \ Onshape Inc
  • Jake_RosenfeldJake_Rosenfeld Moderator, Onshape Employees, Developers Posts: 1,646
    edited July 2017

    I copied your document and if you comment everything out after the first opExtrude it works fine and creates the frame:

    The error I am seeing is:

    Call qCreatedBy(Sketch, EntityType (string)) does not match qCreatedBy(Id, ...)

    Because of line 39:
    qCreatedBy(sketch1, EntityType.FACE)
    should be:
    qCreatedBy(id + "sketch1", EntityType.FACE)

    (qCreatedBy is looking for the feature id, not the sketch object itself)

    If I fix this, there is another issue with your for loop (comparing definition.length with the index doesn't really make sense.  What units would you want the comparison to happen?). It seems like you are trying to compare in inches, so you probably want to do the following:
    for (var i = 0 * inch; i < definition.length; i += 1 * inch)

    Fixing this causes some other issues, but they seem pretty easy to debug (and I'm not sure how to fix them for you because I'm not sure of your design intent).  This is as far as I got:


    Additionally, this may be useful for you:
    If you go to the "monitoring execution information" section of the help document, you can see how to use the 'monitor' feature, which will underline exactly the lines that are causing issues.

    Let me know if there is anything else I can help with.

    EDIT: Ilya beat me to it! Thanks Ilya!
    Jake Rosenfeld - Modeling Team
  • 3966_cad3966_cad Member Posts: 10 EDU
    Thanks so much!
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